working with brass
working with brass
I am relatively new to the CNC world and never posted before. I have made hundreds of things all in 2D, all in wood. I have a design in mind that will use some brass inlay ed in wood. My problem or question is where can I go to get a better idea on tools, feeds and speeds for brass. i could destroy some bits to figure it out but has anyone else tried this?
- TReischl
- Vectric Wizard
- Posts: 4645
- Joined: Thu Jan 18, 2007 6:04 pm
- Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
- Location: Leland NC
Re: working with brass
Well, I do not have it all figured out but do have a few suggestions.
Brass is grabby, will try to pull the tool into it or pull the work.
Doing any metal work on a router is testy. The spindle speeds are typically way too high. Our routers are typically not as rigid as a machine tool. When doing brass and aluminum I have used very slow feed rates, in the neighborhood of 20-25 IPM, sometimes slower for small cutters below .125 dia. Clearing the chips helps a lot. A lot of heat can be generated so if you can have an air line blowing a bit of air it really helps out.
Generally for all metal work I use HSS bits on the router. Couple of reasons, they can be had cheaply these days so when one breaks it is not a big deal, but more importantly they are much sharper.
When doing profile work I use the ramp/spiral option rather than plunging to depth of cut. Usually take about .010 - .015 per pass. Like I said, slowwww.
Another tip is to remove metal using conventional means whenever possible. If you can rough drill a hole, do it. If you have a cut out and have a scroll saw, remove most of the material that way, much faster. If you can rough saw the profile on a bandsaw and still fixture the part, do it that way.
In my shop I run a metal working lathe and mill. Those little machines can cut aluminum, brass, and steel much faster and easier than my router. In other words, most any machine tool is better at it. But boy, can the router come in handy! Later today I need to cut a hex shape in the end of some aluminum round stock to build a die holder for the lathe. So I will rough drill and bore out the piece to waste the bulk and then use the router to create the hex shape.
One other thing, all brass is not created equal. Pay attention to the grade you want to cut, make sure it is free machining.
Brass is grabby, will try to pull the tool into it or pull the work.
Doing any metal work on a router is testy. The spindle speeds are typically way too high. Our routers are typically not as rigid as a machine tool. When doing brass and aluminum I have used very slow feed rates, in the neighborhood of 20-25 IPM, sometimes slower for small cutters below .125 dia. Clearing the chips helps a lot. A lot of heat can be generated so if you can have an air line blowing a bit of air it really helps out.
Generally for all metal work I use HSS bits on the router. Couple of reasons, they can be had cheaply these days so when one breaks it is not a big deal, but more importantly they are much sharper.
When doing profile work I use the ramp/spiral option rather than plunging to depth of cut. Usually take about .010 - .015 per pass. Like I said, slowwww.
Another tip is to remove metal using conventional means whenever possible. If you can rough drill a hole, do it. If you have a cut out and have a scroll saw, remove most of the material that way, much faster. If you can rough saw the profile on a bandsaw and still fixture the part, do it that way.
In my shop I run a metal working lathe and mill. Those little machines can cut aluminum, brass, and steel much faster and easier than my router. In other words, most any machine tool is better at it. But boy, can the router come in handy! Later today I need to cut a hex shape in the end of some aluminum round stock to build a die holder for the lathe. So I will rough drill and bore out the piece to waste the bulk and then use the router to create the hex shape.
One other thing, all brass is not created equal. Pay attention to the grade you want to cut, make sure it is free machining.
"If you see a good fight, get in it." Dr. Vernon Johns
- Bob Jr
- Vectric Wizard
- Posts: 463
- Joined: Thu Aug 13, 2009 2:13 am
- Model of CNC Machine: Axiom, Shark
Re: working with brass
Here's some more information from Vectric's last Users Group Meeting:
https://ugm.vectric.com/session/advance ... -and-brass
https://ugm.vectric.com/session/advance ... -and-brass
"Be accurate."
W. Tell
W. Tell
- Bob Jr
- Vectric Wizard
- Posts: 463
- Joined: Thu Aug 13, 2009 2:13 am
- Model of CNC Machine: Axiom, Shark
Re: working with brass
Popular Woodworking (December 2020 #256) just included an article on routing aluminum and brass with a CNC Router.
"Be accurate."
W. Tell
W. Tell
-
- Vectric Wizard
- Posts: 722
- Joined: Sun Jun 16, 2013 4:40 am
- Model of CNC Machine: Home Built 4-axis Router
- Location: Fort Collins, CO
Re: working with brass
I have done a few projects with brass and found it WAY easier to machine than aluminum. I used the common 360 alloy with some lead content that machines nicely, almost like some super hard hardwood. It does not stick, needs no lubricant or cooling but obviously the feed rate and depth of cut must be reduced to avoid bit breakage for smaller bits. Plunge moves should be ramped but I did not reduce speed (rpm) much. An air jet may help clear chips from narrow cut channels and avoid pulverizing them. Also, brass does not leave sharp swarf on the floor that gets stuck in your shoes.
Dovetail and Finger Joint, Puzzle, Maze and Guilloche freeware at fabrikisto.com/tailmaker-software
- TReischl
- Vectric Wizard
- Posts: 4645
- Joined: Thu Jan 18, 2007 6:04 pm
- Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
- Location: Leland NC
Re: working with brass
Yup, aluminum can be nasty. Gum up on the cutter, snap!
I have only cut brass once on the cnc, it went well. I would love to cut brass a lot more, but the cost, YIKES!
I have only cut brass once on the cnc, it went well. I would love to cut brass a lot more, but the cost, YIKES!
"If you see a good fight, get in it." Dr. Vernon Johns
-
- Vectric Craftsman
- Posts: 232
- Joined: Wed Jul 05, 2017 9:13 pm
- Model of CNC Machine: 24 X 36 3 Axis
- Location: Ipswich, South Dakota
Re: working with brass
I agree that machining brass is much easier than machining aluminum. Both metals need to have very sharp cutters for the best results. I have found that bright finished HSS with a high inclusion angle works best for both. While you can do a descent job on brass with coated bits, coated cutters do not typically work very well at all on aluminum. The main reason being most coatings have some aluminum, AlTiN for instance, in their formulation which causes aluminum to stick to the cutter; unless you are using a coolant formulated for machining aluminum. Aluminum has a nasty trait in its transition temperature between solid and liquid states which causes it to behave like a paste. That property is great for making thin walled aluminum cans, die casting and other forming processes but it is a pain in the butt for machining. High spindle speeds, especially without coolant, cause aluminum to reach that temperature at the cutter interface and stick to the cutter.
Machining any metal works best with spindle speeds much slower than a typical router or 2 pole spindle are capable of achieving. If I were to do metal work with my CNC router to any great extent I would invest in a 6 pole spindle. That would allow spindle speeds slow enough to be more in line with best practices for metal working. An off shore water cooled 80mm dia. 2.2Kw 4 bearing ER20 collet unit can be had for around $900 and on Amazon, a domestically labeled unit is about twice that. That is less expensive than a CNC mill and would allow me to get by.
Ed
Machining any metal works best with spindle speeds much slower than a typical router or 2 pole spindle are capable of achieving. If I were to do metal work with my CNC router to any great extent I would invest in a 6 pole spindle. That would allow spindle speeds slow enough to be more in line with best practices for metal working. An off shore water cooled 80mm dia. 2.2Kw 4 bearing ER20 collet unit can be had for around $900 and on Amazon, a domestically labeled unit is about twice that. That is less expensive than a CNC mill and would allow me to get by.
Ed
-
- Vectric Apprentice
- Posts: 92
- Joined: Tue Apr 04, 2017 11:44 pm
- Model of CNC Machine: AVID PRO4824
- Location: West Kentucky USA
Re: working with brass
I think bronze is the best for carving.
-
- Vectric Apprentice
- Posts: 92
- Joined: Tue Apr 04, 2017 11:44 pm
- Model of CNC Machine: AVID PRO4824
- Location: West Kentucky USA
Re: working with brass
Thanks Todd, I use .02" doc 75 ipm. 20% stepover with an 1/8" 2 flute Carbide upcut for the roughing pass and a .5mm 2 flute tapered ballnose with .5mm doc 50 ipm and 12% stepover finish pass.
24,000 rpm for both, No lubricant and no heat.
My brother works for a monument company and saves me any lawnmower damaged plaques or markers they replace.
I'm working on a foundry furnace to melt down small scraps into 1/4" thick sheets but we'll see how that goes.
24,000 rpm for both, No lubricant and no heat.
My brother works for a monument company and saves me any lawnmower damaged plaques or markers they replace.
I'm working on a foundry furnace to melt down small scraps into 1/4" thick sheets but we'll see how that goes.